CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Needing an approach for using ICEM mesh in FSI

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By backside
  • 1 Post By backside

Reply
 
LinkBack Thread Tools Display Modes
Old   December 29, 2010, 15:50
Default Needing an approach for using ICEM mesh in FSI
  #1
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
Dear Friends,
I am working on 2d FSI problem with ansys workbench. I performed the meshing in ICEM. I know how to import 2d mesh from ICEM to CFX, but in FSI modeling (Oscillating plate in cfx tutorial as reference of modeling) I can't import the mesh. I don't know if it is possible to use ICEM mesh in ansys workbench FSI problem.

Regards,
anno_x is offline   Reply With Quote

Old   December 30, 2010, 12:05
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Workbench Simulation requires the geometry for applying bocos... So you can't just import the ICEM CFD mesh.

However, if you go in thru ANSYS Meshing, you can use ICEM CFD interactive to generate a mesh in ICEM CFD and suck it back into ANSYS Meshing where it is automatically associated with the geometry...

Depending on your needs, you may even be able to get what you want directly from ANSYS Meshing.

ICEM CFD interactive finally got useful at R13, so hopefully you are up to date. Otherwise send an image of your mesh and maybe I can help you get similar in ANSYS Meshing (Workbench)...
PSYMN is offline   Reply With Quote

Old   March 5, 2013, 13:13
Default
  #3
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
Hey,

I'm having the same probelm. I want to create a mesh in ICEm, that afterwards I can use in ANSYS to do a 2-way FSI analysis (workbench).

For that I started with the geometry, which is just made of curves and points. The geometry is a 2D hydrofoil in a control volume. I proceeded with the blocking and defined the mesh params. If I pre-mesh it, everything looks fine. Then I created by premesh>>convert to unstructured mesh the .uns file.
As a last step selected the solver (ANSYS CFX) and wanted to write the file. But then a get this:

Running ICEMCFD - CFX5 Interface Vers. 14.0.0

Error : no volume elements found.child process exited abnormally

It's clear that I shouldn't have volumes as I try to model a 2D Case. Where I have to fix my problem?

Best Regards,
Lukas
backside is offline   Reply With Quote

Old   March 5, 2013, 14:11
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
did you choose the 2d option? is your mesh in x-y plane?
Far is offline   Reply With Quote

Old   March 5, 2013, 14:22
Default
  #5
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
where can I choose this? If it's for the blocking, yes 2D blocking was selected, but my mesh is in X-Z plan. Maybe there is the problem

Last edited by backside; March 5, 2013 at 14:40.
backside is offline   Reply With Quote

Old   March 5, 2013, 15:03
Default
  #6
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
I rotated the geometry and the blocking in the XY-plane. But I got the same error message.
Attached you can find the geoemtry and teh blocking. The mesh is very poor at the moment, I just want to try to import like this before I waste time to create a better mesh..

By the way thanks for your help
Attached Files
File Type: zip 2DXYPLANE.zip (4.9 KB, 4 views)
backside is offline   Reply With Quote

Old   March 5, 2013, 15:11
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Find attached files. Try them...
Attached Files
File Type: zip 2DXYPLANE.zip (12.0 KB, 4 views)
Far is offline   Reply With Quote

Old   March 5, 2013, 15:43
Default
  #8
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
In fact you deletet my solid blocks (the 2 blocks in the blade moved to VORFN) and changed the flow solver from ANSYS CFX to ANSYS Fluent, where now one can choose 2D are 3D mesh. Is this correct? (At least it functions very well to import into Fluent)

But as I do a FSI (fluid-solid interaction) I can't erase the meshing of my hydrofoil. I need it to do a transiant structural analysis (ex. an initial displacmenet or pressure for 0.5secondes). So I have to keep both, fluid- and structure-mesh.
backside is offline   Reply With Quote

Old   March 5, 2013, 21:44
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
In that case you need to change the material to solid . Right click on parts and make new part. Choose the last option (material) and select the blocks inside the hydrofoil and name it solid. Generate unstructured mesh and go to output tab and select "2d" option and you are done.

And now import Fluent mesh (.msh) into cfx-pre and it will extrude mesh by one element. You have now 3d mesh !!!
Far is offline   Reply With Quote

Old   March 19, 2013, 21:29
Default
  #10
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
I found a very good way to do the 2 way FSI.
In the transiant structural, at the model, one can choose as a insert mesh methode a multizone. In the advanced settings one can choose to create a ICEM CFD interactive mesh. (for more infos see: Video sample)

I have done that for the solid as for the fluid part. At the last stage of my settings, one has do define the boundary conditions for the fluid ( control volume) in the Fluid CFX. But there suddenly I have like defaults in my geometry. I checked my blocking as well as the mesh generation, they seem to be correct in ICEM. I even ensured that every face of the blocking is correctly projected on the surface.
Because of these defaults (see attached picture) I can't create the right boundary conditions. At the outlet for example this creates reflow, as the little box (red circle) is also attributed to the outlet...

Why I got these defaults? Could it be an error because of tolerances between ICEM and Workbench?
Attached Images
File Type: png setup.png (76.4 KB, 19 views)
Azy likes this.
backside is offline   Reply With Quote

Old   April 10, 2013, 22:10
Default
  #11
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
backside is on a distinguished road
I could manage my problem with the mesh creation.

Initialy you start from the basic 2-way setup with a part for the solid (Transiant structural) coupled with the fluid (CFX). You can create or import a geomtry in Design Modeller after making/choosing the material. Then it comes to the meshing (Model for structur, Mesh for Fluid). The approach is for both the same, so I will explain the procedur for the solid part.

1.Double Click Model, so that Mechincal is opening.
2.Geometry-Hide the body you dont use. Check if right material is associated.
3.Mesh - Insert Method - MutliZone. There select advanced options. Now you can choose Write ICEM CDF Files: Interactive , ICEM CFD Behavior: Postprocessing.
4,Update Mesh. Now ICEM should open. Sometimes it is usefull to create a script (Link in further post). Be carrefull: When you create your own blocking it must have the same name as before to be regognized by Workbench (Usually it is called CREATED_MATERIAL).
5. When the premesh is done->export mesh as unstructured block.

Note: I changed the triangulation tolerance (ICEM-Settings-Model-Triangulation-Tolerance) to get rid of my mesh default of the further post

That's it.

Hope this will help you
Azy likes this.
backside is offline   Reply With Quote

Old   April 12, 2013, 03:57
Default
  #12
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
If you´re using ANSYS 14.5 you can use an extra ICEM-Meshing container within the project schematic. It makes the whole scripting/blocking/updating process way more flexible and accessible.

Matthias
mvoss is offline   Reply With Quote

Old   April 13, 2013, 09:36
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
an extra ICEM-Meshing container within the project schematic
where it is located ?
Far is offline   Reply With Quote

Old   April 16, 2013, 03:31
Default
  #14
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
sorry for the delay.
The icem-container is.... at least in my installation, right below the Geometry component system.
I think it strongly depends on the licences you´ve got.
mvoss is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
converting ICEM mesh to OpenFOAM bmikuz OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 8 May 2, 2013 10:55
FLUENT - ICEM / Segmentation Violation Error (Hybrid Mesh) Joachim ANSYS 2 March 24, 2013 08:35
Unstructured Mesh ICEM on a cube jerome_ ANSYS 0 May 30, 2012 05:34
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Hex-Tet Mesh Merge in ICEM Tristan CFX 1 September 26, 2008 05:40


All times are GMT -4. The time now is 03:43.